Thanks. I figured there was a way to do that. That makes things so much neater.
Further to this,
Maybe if you want to display more info than what the default cutlist gives you, it is possible to assign any property you want to your cutlist properties and add it as a column to your indented BOM.
Right click the weldment symbol in your tree and choose "properties"
then you can add a property to all cutlist items simultaneously, such as Part Number or Weight. But literally anything you want! Then click OK.
Now when you look in the cut list properties we have a new WEIGHT property for each item, and i've made it display the mass calculated by solidworks. Alternatively you could manually type in information if it couldn't be generated as a special Solidworks property.
I can then simply add this as a column to the indented BOM in the drawing,
to add a new column, right click a column and choose insert > column right / left
you are then prompted for a property to populate that column with. It could be a custom part property that applies to your entire part file. Or we can choose Cut List Property,
then from the second drop down you can choose your new property,
don't forget you can save table templates so you don't have to keep adding and removing columns every time.
simply right click the table and choose save as, then save it wherever you want, generally best saving in the filepath all your other table templates are stored.
That is some deep dive wonderfulness right there. I am going to have to explore those possibilities. Thanks!
Is it possible to add these properties using the property tab builder? What you have shown would be very helpful and may make me look at weldments again as I would finally be able to have a standard appearing BOM with them.
I have not had luck using property tabs for weldment cut list items. You can make the property tabs, but there are issues with text expressions getting replaced with actual values (SPR 631734) when you choose APPLY.
I think the best way for this would be to have a part template that already has your usual cut list properties assigned.
Have an empty part file open (with your preferred document properties all set).
hit the weldment button on the Weldments tab so that it appears in the design tree.
similar to above, right click the weldment icon in the tree and add all your additional preferred cut list properties.
leaving blank the ones that would differ from item to item. But using SW properties where possible to drive the value. (Eg weight driven by SW-Mass)
Remember you can add your own manual ones. (Eg, Spares Kit in my screenshot below)
Then if you save this part as a template, you can use this template any time you want to start a weldment part with your preferred custom cut list properties all ready to go.
File > Save As > Part Template.
Be sure to save it in a location that Solidworks knows about in System Options > File Locations > Document Properties